I made a decision to master this tool and it has really paid off. I just learn something new every day by reading through the forums, blogs, SolidWorks LinkedIn groups and by watching Youtube videos. I also optimize my setup by adding shortcuts, mouse gestures (working on it) and demanding a 3D mouse!

Can't wait to hear what other have to say. I'll add items to my list when I think of them.

Reading blogs and the forums

Using a 3D mouse, even the simplest one is a big improvement over just a mouse

Adding X, Y and Z axes to your part and assembly templates

Move the basic toolbars to the left (and turn off Use Large Buttons with text) of the screen to maximize screen space on widescreen monitors

Scrolling in the command manager instead of clicking

Holding alt while dragging drawing views so you don't have to click the edge

Adding Page Up and Page Down to scroll through drawing sheets!

Using the F key to fit the model/drawing on the screen

Select two parts/assemblies, then click the mates tab in the feature tree to see the mates between them highlighted

Search using the top bar of the feature tree

Creating macros for tasks that can easily go wrong, that take a long time or that you don't enjoy doing

On the topic of macros: killing those that are stuck in an infinite loop with Ctrl + Pause-Break

Customizing the crap out of SolidWorks, even though no one can work with your pc anymore. I even added a custom shortcut to open the customize window

Using Alt and Control when clicking up/down in dimension boxes, it changes it 10 and 0.1 times the default amount.

My main one since 2008 when it was introduced is to define your S key for your Sketch, Part, Assembly and Drawing needs.

Also, when you're dimensioning at the part level, add dimensions to entities as far up the FeatureTree. Keeps the amount of Parent/Child relations down to a minimum which allows more freedom in moving entities up and down the tree.

Lastly, if you have more than 1 user, get yourself a PDM tool (SolidWorks has a few really good ones ). Duplicate files, renaming files, moving files, etc. will drive anyone nuts.

We recently added the axes X, Y and Z to our part and assembly templates as well. No more linear patterns linked to feature edges so no more broken patterns. It's a real improvement, I'll add it to my previous post as well.

Attachments

I wouldn't really say that anything I do is a "trick" but I do employ several practices with specific goals in mind that make things easier long run.

My main goal when making a model is to make the model flexible, adaptable, understandable, & simple.

1. I try and use constraints over dimensions whenever possible

a. This helps with making multiple configurations of my models as I only need to change 1 or 2 dimensions for a new configuration instead of 20. Also makes making revisions less likely to break the model tree

2. I try and create my 3D models with feature relations that make sense. I also make use of reference geometry to avoid bad relations

a. This is of course subject to what you are designing but generally if you follow a standard feature ordering you won't get that important feature accidentally related to that random fillet that you decided to delete and destroys half the model tree.

3. I try and name features and use folders in my models so that if another person needs to work with my model they can easily locate everything and make changes where needed.

a. In my opinion if things are understandable and easy to change people are more likely to change features instead of tacking them on at the end of the model tree.

4. I try and use as few models/features/relations as possible while still fully defining my models.

a. This one is rather self-explanatory but if you can make a feature with one sketch instead of ten it's probably better to do it that way. Granted there are times when this can be broken but as a general practice it's better.

b. I use models with configurations so as to avoid having multiple models with small variants. Design tables, & equations can accomplish this as well but I find for others looking at my models configurations are the most intuitive.

5. I use custom properties in my models and have these same properties auto populate my drawing template title blocks.

a. This is mainly a time savor and error prevention as it ensures all drawings generated from the model have consistent information.

Like I said none of these are really "tricks" but I find by following these practices when making my models everything ends up running smoother long run. Basic rule I'd say is "think before you model".

Why is the 'height' plane not divided into three planes just like the other planes are? You know, so you would have perhaps 'bottom', 'height middle' and then 'top'. Whereas currently you have only the two 'floor' and 'top'. Or am I missing something? (Probably) lol

I don't think this counts as a trick, but the main thing that I utilize every day is my experience as a Tool maker & a fabricator.

Thinking about every part I designed from the standpoint of "How would I make that" has helped me throughout my career as a designer.

And while people working with me or for me in my department may not have that kind of experience, I encourage them to spend some time on the floor whenever possible. Talking to and watching what the tool makers we have here are doing.

I truly believe it is something that is missing in the process for some people I have worked with over the years.

Other things I utilize are:

#TASK

Top down modelling

In context assemblies(Non circular BTW)

Virtual parts/assemblies

Spell check. J/K

Property tab builder

Multi body parts(Both welded and bolt together) This creates sub assemblies that are easy to manipulate.

I am sure there are other things as well, but these are the bulk tools that I think help me in my every day design and concepts.

Just as a question. If you are making multiple parts that will fit together do you define your planes just based on each individual part or so they work together?

I always like to make my planes so that when I go to make my assembly almost every constraint is either a coincident or symmetric constraint about the main 3 planes whenever possible.

~Eric

I try to keep in mind how I'm going to be using the Parts in the Assembly when I model them, but I use all different types of mates. Some of my assemblies are well over 150' long, so it would be a nightmare trying to model everything so I could mate to the main planes only.

Others have already listed my primary favorites, so I'll just add one. Or is it two?

Advanced Component Selection (my keyboard shortcut set to CTRL-SHIFT-A, yet no default shortcut) is greatly helpful in determining the error-generating mates when revising a complex assembly. Before finding this, it was like the proverbial needle in a haystack to figure what to suppress in order to repair an assembly.

Similarly, using Axis when relevant for parallel mates instead of a plane (ref. Peter Brinkhuis's earlier post) often allows for more flexibility for change while maintaining design intent. This often avoids the errors I used to repair with Advanced Component Selection above. Avoid Perpendicular forever (with exception of Profile ref. planes on a Sweep) because Perpendicular mate cannot use Flip Mate Alignment, and it's more useful to use Parallel or Coincident mate with well defined reference planes & axes. “An ounce of prevention is worth a pound of cure,” as Benji Franklin said.

One more that I just thought of. When placing the first component in an Assembly, I first of course choose the component, but then I click on the green check mark at the top of the "Insert Component" PropertyManager. That fixes it with it's three primary planes aligned with the same planes in the Assembly instead of the more or less random placement you get by clicking in the graphics area.

I search for the proverbial needle as well and looked at the command Advanced Component Selection. I can't figure out how you use this to aid in repairing assemblies that that go haywire. Can you expand on how this is used?

Glad to expand, Rick. I mostly used Component Status criteria queries, when assessing components within an assembly.

1 _ Component Status _ = Has Mates - Over Defined

2 Or Component Status _ = Has Failed Mates

Isolate Selection.

Narrow the haystack into a handful, and investigate a smaller subset. Suppress mates and poke the smaller beast with sticks until it plays nicely with others.

Narrow it further with (bad mates above +) = Fixed or not= Fixed, by what works in situation. EDIT: As you narrow to the issue by resolving some items, Repeat steps above to re-filter out the 'good'.

Another additional criteria or alternative in a separate situation is:

1 _ Component Status _ = Has Errors

2 Or In Context Relations Has broken external references is yes

especially if I've recently suppressed or deleted something that I didn't know something else was referencing (breaking sketches, then features, and then even more references or mates .. the downward spiral to madness).

Other variation is not= Fully defined, if you're looking to firm up a starting design. That's a different sort of detail chase rather than chasing down the bad mates.

If all hell has broken loose, combine more criteria by stacking one on to another, or use "And" instead of "Or" to keep narrowing the pile. "And" boolean with multiples will get you to the items that fail in multiple ways, because.. dang why did I do that in the first place. Maybe I ought to revert the file to a previous version (bi-daily Server backups or archive copy) instead, because undo doesn't work anymore and I really did it this time.

I used to have these saved out as favorites, but lost them in an upgrade to 2016 IIRC, and honestly haven't needed them much since. I think it was mostly due to changing the way I mated components, not the software upgrade, that alleviated my need for this power tool. It's still critical, though, in examining someone else's mish-mosh that didn't follow my logical preferences to begin with, as in contractor work.